Is it Simultaneous Switching Noise or Crosstalk?

With the multitude of signal integrity problems that can arise in real PCBs, how can the astute designer distinguish them all? Some problems are clearer than others, with specific signal integrity measurements being developed for testing and measuring particular aspects of signal behavior.

One question that arises has to do with the appearance of a fluctuation in the output voltage on a banks of I/Os, known as simultaneous switching noise or, more popularly, as ground bounce. If you examine the voltage induced when multiple outputs switch simultaneously, this type of potential fluctuation looks a lot like inductive backward (i.e., near-end) crosstalk. The fact is, multiple signal integrity problems could be present on a single interconnect simultaneously. So how can you distinguish between the two properly and determine whether your layout needs a change? Let’s break down the two effects and determine which is having a greater impact on signal integrity.

What is Simultaneous Switching Noise?

I’ve seen IC designers typically use “simultaneous switching noise” while PCB designers tend to more often use “ground bounce” to describe the same phenomenon. Simultaneous switching noise refers to an apparent change in the ground plane potential near a switching IC. In reality, the ground plane potential in the PCB has not changed, rather a potential has developed between the PCB ground plane and the package die ground plane.

This is a parasitic effect that arises due to pin-package parasitic inductance. In an ideal IC, the bond wire, lead frame, and any copper connecting the ground pin to the PCB ground plane are perfect conductors with zero inductance, but real PCBs don’t behave in this way. When the IC switches, the parasitic inductance in these elements (all of which can be taken in series) develops a potential that opposes the rush of current between the PCB ground plane and the I/O buffer circuit on the semiconductor.

The typical circuit model used to understand these parasitics is shown below.

• Learn more about ground bounce in this article

Because the ground plane is the reference for the output pin and the die, there must be a nonzero voltage between the driver’s die ground plane and the PCB ground plane, whereas the receiver is referenced to the PCB ground plane. Take a look at this article for more information on ground bounce.

If you look on an oscilloscope trace tracking the output from an I/O, it can show ringing due to current being sunk along the above path. When multiple I/Os switch simultaneously, they are effectively drawing from the same I/O power supply in parallel. Effectively, the back EMFs generated from multiple I/Os superimpose on a victim I/O due to the raised ground potential measured near the victim. The result is typically an underdamped ringing waveform.

How can this ringing be reduced? The reasons this occurs are as follows:

• Insufficient decap and/or bypass capacitance on the I/O power supply
• Insufficient damping along the current path along the I/O buffer
• Excessive inductance along the GND trace and GND return path
• Excessive inductance along the bypass capacitance path

Normally, we reduce the inductance by using a GND plane (reduce spreading inductance) and providing a direct trace path to any GND connection. We then make sure the connection to the bypass capacitor is also short so that there is no inductance along that path.

The use of a series resistor for damping is typically not used in a high-speed channel, the reason being that the edge rate gets too slow and too much power is lost across the resistor if you aim for critical damping on the edge. It can be used on slower baud rate buses with fast edge rate, like SPI, because those buses do not need the fast edge rate and they do not have an impedance specification.

Comparing with Backward Crosstalk

If you measure the output from a poorly-bypassed component, the voltage fluctuation seen at the output resembles a signal that looks like a voltage/current spike due to inductive NEXT. The problem in distinguishing the two is related to parasitics:

• Real ground planes and return paths from ICs have parasitic mutual inductance and resistance. In other words, they can pass crosstalk between each other, just like a pair of signal traces.
• If an IC is not decoupled from the ground plane, the voltage produced by NEXT and ground bounce can be similar as the parasitic inductances tend to be similar in magnitude and polarity.

The second point I mentioned is the reason bypass capacitors are used near ICs with high output pin count/fast rise times/strong current draw. Just like with decoupling capacitors in PDNs, a bypass capacitor used in this way does not decouple or bypass anything. Instead, it just provides a reservoir of charge (and voltage) that compensates for ground bounce or any other voltage fluctuations seen between the output and ground.

Here, I’ve shown an overdamped response in NEXT and FEXT, but any of these signals can exhibit ringing if parasitic self-inductance is high. Although the ground bounce waveform occurs in an equivalent RL circuit, it can also exhibit ringing due to stray capacitances; this generally occurs with CMOS components. Furthermore, the damping experienced by these signals will depend on the load impedance. As these signals can be quite dramatic, they can cause unintended switching in the receiver if the noise margin is thin.

How to Distinguish Simultaneous Switching Noise and NEXT

This can be a difficult task, especially when working with a prototype board that has some signal problems. The key is to try and separate the effects of crosstalk and simultaneous switching noise. The standard configuration for measuring ground bounce is to wire an isolated conductor (a coax cable is ideal) from a load component directly to a meter, which is held at the same ground potential as the driver and receiver. Hold the driving output on this pin LOW, and drive all other outputs on the driver. This provides a direct measurement of ground bounce, but this configuration still has a problem in that the LOW trace is still susceptible to crosstalk.

Thankfully, there is a better way to do this. Howard Johnson recommends doing this by cutting the suspected victim trace and wiring up a coaxial cable with matched impedance directly from the driver and the receiver, and measure the signal entering the coax. The coax will be shielded against crosstalk, allowing you to measure voltage fluctuations due to ground bounce alone in this conductor. This measured voltage will be seen by all other switching outputs, whereas any voltage fluctuation from crosstalk will vary across all the traces. Note that, in this configuration, the driver output connected to the coax should also be held LOW while the remaining I/Os are driven.

When you do measure some variation in the output from an IC and you suspect ground bounce is excessive, perhaps the easiest check is to swap your bypass capacitor for a larger capacitor. The bypass capacitor will not affect the crosstalk signal, but it will affect the ground bounce signal. If you increase the bypass capacitance and the voltage fluctuation does not change significantly (or there is no change at all), you know strong ground bounce is not the source of the problem.

With the post-layout simulation and crosstalk analysis tools in Altium Designer®, you can easily simulate crosstalk in your layout and use this as a reference for further measurements. These results can be used as a reference for test and measurement results, which helps you verify whether simultaneous switching noise is creating major problems in your board. You’ll also have access to a broad range of tools for circuit simulations, managing component data, and preparing for production.

Now you can download a free trial of Altium Designer and learn more about the industry’s best layout, simulation, and production planning tools. Talk to an Altium expert today to learn more.